When solving typical task, such as structure with bolts, I can’t determine stress in the beam elements. When running inp file at pre-processor, I can see beam elements in the mode. When starting .frd, beams are disappear. *EL PRINT is not working for beams.
The example: pret3.inp, all versions.
How I can solve it?
CalculiX CrunchiX User’s Manual → *PRE-TENSION SECTION:
For beam elements a linear multiple point constraint is created between the nodes belonging to the beam element. The beam element itself is deleted,i.e. it will not show up in the frd-file. Therefore, no other boundary conditions or loads can be applied to such elements. Their only reason of existence is to create an easy means in which the user can define a pretension.
Thank you. But bolt force is the main result in this case. How I can get it for deleted element?
пн, 3 апр. 2023 г., 17:34 Calc_em via CalculiX <notifications@calculix.discoursemail.com>:
try read pret3.inp nam in the terminal after loading .frd however you need to create results for the elements using *EL FILE or *ELEMENT OUTPUT. Otherwise check your results at pret3.dat file. Do not forget the different behavior of beams when using parameter OUTPUT=3D (default) or OUTPUT=2D.
Thank you, but
beam results are stay zero at frd or dat.
you have to request them; in pret3 example they’re not requested. the pret3 input deck part requesting output follows:
*STEP
*STATIC
*CLOAD
99,1,1.
*NODE PRINT,NSET=Nall
U
*NODE PRINT,NSET=Ncoup1,TOTALS=YES
RF
*NODE PRINT,NSET=Ncoup2,TOTALS=YES
RF
*END STEP
you have to request stresses or whatever you need, from all elements or the beam elements in particular.
Hello Juan,
I mean, there are no results for beam at .frd file, as well as beams are eliminated
When you read/add inp, you are not obtaining results, just adding input to output
But
*NODE PRINT,NSET=Ncoup1,TOTALS=YES
RF
*NODE PRINT,NSET=Ncoup2,TOTALS=YES
RF
may be the answer. If I can get forces at the ends of bolt, the problem is solved
Regards
OK. now I see what you mean, my mistake. According to the manual:
Internally, the nodes belonging to the element face surface are copied and
a linear multiple point constraint is generated between the nodes expressing
that the mean force is the force specified by the user (or similarly, the mean
differential displacement is the one specified by the user). Therefore, if the
user visualizes the results with CalculiX GraphiX, a gap will be noticed at the
location of the pre-tension section.
For beam elements a linear multiple point constraint is created between the
nodes belonging to the beam element. The beam element itself is deleted,i.e.
it will not show up in the frd-file.
The other problem, from what I’ve found from calculations,
this structure is not really bolted connection.
It has certain pretension force between 2 node sets and keeps it
constant during loading, what is not completely right.
I have to find the way how to keep bolt deformable at all steps, so it
is really works as axially preloaded beam between to parts.
Regards
Hello Juan
Probably *PRE-TENSION card is not the best option because it keeps preload constant at all steps and removing bolt
in this case doesn’t mater bolt diameter and material.
Is there other option to create preload? Maybe the temperature or some kind of initial strain?
*BOUNDARY, FIXED has to be used for that DOF in the second step to freeze preload so that the beam can deform normally due to actual load. At least that’s what needs to be done for 3D solid models of bolts and in software other than CalculiX in which beams are deleted. But you should still be able to apply BCs to the reference node in the second step.
Hello,
*BOUNDARY, FIXED
should it be applied within 2nd step?
how to apply it just to the bolts?
For example at the first step I have initial deformation =0.001
*BOUNDARY
3102,1,1,0.001
does it mean that second step should have
*BOUNDARY,FIXED
3102,1,1,
?
Yes, the boundary condition used for pretension in the first step needs to be removed and replaced with a fixed one in the second step.